9 Replies Latest reply on Nov 5, 2014 9:18 AM by aclark

    Update/replace cached symbols in DxDesigner

    aclark

      I seem to be having some problems with a few "link" symbols in DxDesigner.  The symbol names are in CAPITALS in the library (e.g. CON_INTER_O.1), but are cached in the schematics in lower-case.  This seems to cause a problem with JUMP TO not working, and causes lots of errors, particularly DRC-121.  I should say that this is EE7.9.4u6, with a shared common central library.

       

      Adding a new link doesn't work - it gets the same lower-case name (I guess the tool notices that the symbols is already in the design, so doesn't actually copy it from the library).  I had a quick look with library services, but I couldn't find an obvious way to access the locally cached symbols like was possible with DC.

       

      A new project created from scratch does not have these problems; however what I'd like to do is fix my existing project, complete with it's 76 pages of schematics and 3000+ components.  We've seen this once before, and in this case, the design was half re-input from scratch because it was a small project and didn't use too many instances (which make copying blocks easier).

       

      Have I missed something else?  How can I force DxDesigner to re-load the symbols from the central library?

        • 1. Re: Update/replace cached symbols in DxDesigner
          robert_davies

          There is no mechanism to force an update of cached symbols in the design, the only way to force a change is to update the symbol definition and perform a symbol update. But DxDesigner is case insensitive/case preserving so this may not get you around the issue you are seeing. A couple of possibilities are either to replace the link symbols with a different symbol with the same graphics, or possibly to add both symbol definitions to your DRC-121 settings (though I've not tried this so it may not see any difference if you list Libname:CON_INTER_O.1 and Libname:con_inter_o.1).

          • 2. Re: Update/replace cached symbols in DxDesigner
            agxinmj

            hai

                   i had the same problem in jumpto i did the following to solve this

            1.configure the link symbol in links in the setup -settings window,input output,bidirectional ,power ports gnd ports

            2.then select automatically propagate net names  through ports in advanced settings 

            3.now reopen the schematics

            4.ensure the net name in the net and the net name in the link symbol are same

            5. if not just disconnect the link symbol and connect it to the net again

            6.net names now will be updated with the link symbol

            7.now click on the link symbol select jump to it shows the list of pages the net is connected you can jump to the corresponding net 

            8.If any problem mail with snip i will help you

            regards

            AGXIN

            • 3. Re: Update/replace cached symbols in DxDesigner
              agxinmj

              hai

                       to update dx designer catche

              1.open the library manager in the dx designer window there will be option to update dx designer catche

              2.if you select update symbols in dx designer the symbol attribute change in central library will automatically get updated

              3. to experience the mismatch go to settings under display settings set the colour for mismatch match and set flag outdated symbol in advanced settings

              4. if the symbol in dx designer is differing in any property that is defined for the symbol in central library then the symbol will be flagged

              regards

              AGXIN.J

              • 4. Re: Update/replace cached symbols in DxDesigner
                aclark

                I wondered about updating the symbol to get a .2 version.  This would also require every other project to update the symbol, which is a little bit of work.  However, I wasn't sure if this would case DxDesigner to change the symbol name, or just increment the version number!

                 

                We changed the settings for DRC to lower-case, and it seemed to solve the DRC errors.  Also changing the library names to lower-case in speccomp.ini solved the linkto problem.  DxDesigner is definately CASE SENSITIVE forDRC-121 and the "linkto" funcionality.  For this specific project, we have made local copies of these files, rather than changing them in our common area because we didn't want to make the changes in all projects.

                 

                Tracing the origin of the problem, this particular design was migrated from DC.  In the DC project and in the DC central libraries, the symbol names are in upper-case.  However, the backup we have of the output of the migration tool shows the symbols with lower-case names.

                 

                We devised a way to correct it by starting a new DxD project, placing the symbols from the cemtral library (therefore copying them into the local DxD cache), and then copying in the blocks and schematics from the project with the problem.  This did solve the lower-case / UPPER-CASE problem, but in the end we had to abandon it.  The new project needed some work because the refdes suffix was applied a 2nd time, and the CES definitions were missing.  However the killer came trying to attach the new project to the PCB.  Many PCB netnames of instantiated blocks ended up with different suffixes compared to the original, and when doing a forward annotate many components in one instance were swapped with parts from another, and thousands of nets disappeared from the PCB.

                 

                In the end, we will have to live with this one project having its own "central" settings that are different to all the others.

                • 5. Re: Update/replace cached symbols in DxDesigner
                  aclark

                  Hi agxinmj.  Thanks for your input.

                   

                  Unfortunately in this case, libman didn't do anything.  The names of the symbols in DxDesigner didn't change to upper case as they are in the library, nor were the symbols flagged as out of date, not was the option to update the symols appear.

                   

                  Our work-around so far is to run this project outside of our centralised set-up, with its own lower-case version of the symbols.  We still have some verify errors reported, but they are manageable, and can be manually checked. (Before there were >1000 errors reporting nets connected without links).

                  • 6. Re: Update/replace cached symbols in DxDesigner
                    agxinmj

                    hai

                                In my library also the name of page connector is in capital and the dx data book it is small but still links working for me ,can you please provide some images about your problem

                    1. when you connect a page connector to a net,click on the page connector properties and see whether the net name is added to the link (page connector ) in the properties window  ,if it is not added first you have to fix this then only links will work

                    2.so for the link which are not jumping click and check whether the net name is updated in the connector

                    1.configure the link symbol in links in the setup -settings window,input output,bidirectional ,power ports gnd ports

                    2.then select automatically propagate net names  through ports in advanced settings 

                    3.now reopen the schematics

                    4.ensure the net name in the net and the net name in the link symbol are same

                    5. if not just disconnect the link symbol and connect it to the net again

                    6.net names now will be updated with the link symbol

                    7.now click on the link symbol select jump to it shows the list of pages the net is connected you can jump to the corresponding net 

                    8.If any problem mail with snip i will help you

                    regards

                    AGXIN

                    • 7. Re: Update/replace cached symbols in DxDesigner
                      aclark

                      One problem is this:  The name of the symbol in the schematic must exactly match the case of the name of the symbol in verify.ini

                      If this is not the case, then verify (DRC-121) will not recognise the links as link symbols and will flag an error for every net used (e.g. CON_INTRA.1 does not match with con_intra.1).

                       

                      Another problem is this: The name of the symbol in the schematic must exactly match the case of the name of the symbol in speccomp.ini

                      If this is not the case, then "jump to" will not appear in the context (right-click) menu.  Curiously, alt-click still appears to work.

                       

                      It doesn't matter what the case is in the library (I don't know about DxDatabook - I place the symbol using the special component button).  What matters is the case that the symbol has in DxDesigner.

                       

                      Note that all links have the same name as the net.

                       

                      In this instance, the problem was caused by the DC2DXD migration tool changing the symbol name from upper case to lower case.  The only solution we have found for this is to have local copies of verify.ini and speccomp.ini in this particular project, that are customised to have the symbol names in lower case (Or normal workflow has these files centralised and the same for all projects).

                      • 8. Re: Update/replace cached symbols in DxDesigner
                        robert_davies

                        Does adding the symbols twice, once in upper case and once in lower case to the DRC settingsand speccomp.ini files solve the issue?

                        • 9. Re: Update/replace cached symbols in DxDesigner
                          aclark

                          We didn't try this; we only changed the case for each of the symbols that was affected, and in that way solved the problem locally in the project.  I'm sorry to say that once the problem was solved, we stopped looking at it; although at least I did at least post the final solution here.  I will see if I can test your idea later.

                           

                          I think that the SPECCOMP.INI file may also be used to generate the list of special components to place, and that maybe putting the symbols in twice may result in them appearing in the place special components drop down list twice, but I don't know.